Imopsing profile at inlet in initial solution for turbomachinery

vishwasvemra · April 21, 2018, 10:15

Hello all,

I am trying to do a computation of an axial compressor in fine turbo, with imposed inlet circumferential pressure profile. I have imposed the profile at inlet successfully, but each time the solver exits with error message of "this type of profile x,y is not yet implemented in the initial solution for turbomachinery ".
I am not able to find an option to put a profile at intial solution. I tried with both a constant value and with radial equilibrium, but both of them exits with above error.
I have checked in manual, and it says that '2D profiles at the main channel entrance and exit are not supported', but i am not sure then, why does the solver exits with this message.

Could anyone please help on this.

Thankyou very much!!

Kind Regards
Vishwas

DarylMusashi · April 21, 2018, 14:30

Dear Vishwas,

are you really sure you correctly defined the profile? The error message ""this type of profile x,y is not yet implemented..." might mean that you used x and y coordinates instead of r and theta. Might this be the case? Please have a look at my attached figure.
May I ask if you have already worked through the manual (FINE™/Turbo > User Guide > File Formats > Files Used as Data Profile)?

Kind regards,
Holger

vishwasvemra · April 21, 2018, 15:05

Dear Holger,

Yes, I think I have imposed the profile correctly. I have checked with the manual, and the data i have is for x,y and p value. So I used first line as 'FINE profile file', then 51 1000(as manual says 51 for x and y and I have 1000 data points) as the second line, after this x y and p values. I could see the imposed profile in viewer window(without any error).
I checked with manual, it says for r theta profile, it has to be structured in proper style of increasing theta order. But I have x-y profile, which I imposed directly. (see attached)

Just for your information, when i impose constant value as initial guess, the solver starts but exits with negative pressure and density.

I have attached the message snapshot.
I think the error is in the initial solution menu, as error message says, not at inlet implementation.
Thanks alot!!

Kind Regards
Vishwas

DarylMusashi · April 21, 2018, 16:19

Dear Vishwas,

in one of the FINE/Turbo tutorials (Aachen turbine) you have to define an inlet boundary profile (1D) as function of r. Often beginners forget to switch from "function of x" (default) to "function of r". In this case the same error message appears, mentioning an issue about the turbo machinery initialization. The real reason is that a "profile along x" is simply not supported as boundary condition.

It might be the solution to convert the X-Y coordinates to r-theta coordinates. You can do a test with a simplified profile just to check if this will work.

Kind regards,
Holger

vishwasvemra · April 21, 2018, 17:18

Dear Holger,

I have tried a simple pressure profile of the r-theta and pressure value. In this profile I have given 12 theta position. For each theta, r and p values are defined. I have attached the file, which I am using for input(for sake of uploading i have changed extension to .txt from .p).
I still get the same error. This time it says r-theta error instead x-y.(attached).

I am not sure why does it says error in initial solution.

Thanks!!

Kind Regards
Vishwas

DarylMusashi · April 21, 2018, 18:33

Dear Vishwas,

the combination 2D profile with turbo machinery initialisation doesn't seem to work independent of the chosen variables (just did a short test case on my side), just as stated in the manual.
But in my case the computation starts successfully with a 2D profile (Total Pressure at inlet, r-theta) when using "constant values" instead of turbo machinery initialization. Could you check that again, maybe you forgot to save the .run file after you changed the initialization to "constant values"?

Kind regards,
Holger

vishwasvemra · April 26, 2018, 12:59

Dear Holger,

Thanks alot.
It does work as you have stated. In my case some issue was coming with constant initial solution. So to get rid of this, i ran a case with uniform inlet flow and generated an initial solution. With this solution, i initialized profile cases and it works fine.
Just for the information, xy profile also works good.

Many Thanks!!

Kind Regards
Vishwas

April 21, 2018, 10:15	Imopsing profile at inlet in initial solution for turbomachinery	#1
vishwasvemra New Member Vishwas Verma Join Date: Mar 2016 Location: Mumbai India Posts: 25 Rep Power: 10	Hello all, I am trying to do a computation of an axial compressor in fine turbo, with imposed inlet circumferential pressure profile. I have imposed the profile at inlet successfully, but each time the solver exits with error message of "this type of profile x,y is not yet implemented in the initial solution for turbomachinery ". I am not able to find an option to put a profile at intial solution. I tried with both a constant value and with radial equilibrium, but both of them exits with above error. I have checked in manual, and it says that '2D profiles at the main channel entrance and exit are not supported', but i am not sure then, why does the solver exits with this message. Could anyone please help on this. Thankyou very much!! Kind Regards Vishwas

April 21, 2018, 16:19		#4
DarylMusashi Senior Member Holger Dietrich Join Date: Apr 2011 Location: Germany Posts: 174 Rep Power: 15	Dear Vishwas, in one of the FINE/Turbo tutorials (Aachen turbine) you have to define an inlet boundary profile (1D) as function of r. Often beginners forget to switch from "function of x" (default) to "function of r". In this case the same error message appears, mentioning an issue about the turbo machinery initialization. The real reason is that a "profile along x" is simply not supported as boundary condition. It might be the solution to convert the X-Y coordinates to r-theta coordinates. You can do a test with a simplified profile just to check if this will work. Kind regards, Holger Last edited by DarylMusashi; April 21, 2018 at 18:06.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Suppress twoPhaseEulerFoam energy	AlmostSurelyRob	OpenFOAM Running, Solving & CFD	33	September 25, 2018 18:45
Segmentation fault when using reactingFOAM for Fluids	Tommy Floessner	OpenFOAM Running, Solving & CFD	4	April 22, 2018 13:30
pimpleDyMFoam computation randomly stops	babapeti	OpenFOAM Running, Solving & CFD	5	January 24, 2018 06:28
High Courant Number @ icoFoam	Artex85	OpenFOAM Running, Solving & CFD	11	February 16, 2017 14:40
SLTS+rhoPisoFoam: what is rDeltaT???	nileshjrane	OpenFOAM Running, Solving & CFD	4	February 25, 2013 05:13

April 21, 2018, 18:33		#6
DarylMusashi Senior Member Holger Dietrich Join Date: Apr 2011 Location: Germany Posts: 174 Rep Power: 15	Dear Vishwas, the combination 2D profile with turbo machinery initialisation doesn't seem to work independent of the chosen variables (just did a short test case on my side), just as stated in the manual. But in my case the computation starts successfully with a 2D profile (Total Pressure at inlet, r-theta) when using "constant values" instead of turbo machinery initialization. Could you check that again, maybe you forgot to save the .run file after you changed the initialization to "constant values"? Kind regards, Holger

April 26, 2018, 12:59		#7
vishwasvemra New Member Vishwas Verma Join Date: Mar 2016 Location: Mumbai India Posts: 25 Rep Power: 10	Dear Holger, Thanks alot. It does work as you have stated. In my case some issue was coming with constant initial solution. So to get rid of this, i ran a case with uniform inlet flow and generated an initial solution. With this solution, i initialized profile cases and it works fine. Just for the information, xy profile also works good. Many Thanks!! Kind Regards Vishwas